Analog fault simulation using Spectre

Hi,

I want to use spectre (from command line) for analog fault simulation.
I have a spectre netlist file (e.g. input.scs) which contains some
values in terms of parameters. (e.g. R1 = 1000*a, C1 = b*1e-6) Now i
want to have a file which will have the fault list(e.g. a=1 b=1, a=1.5
b=1, a=1 b=1.5, a=0.8 b=1.2 ...) Spectre should take this file and
simulate the same circuit (input.scs) the required number of times,
each time taking the specified set of values of a and b.

Is this possible, and if yes, how? I am using spectre 5.0.

 

what you are describing is called "parameters" in spectre jargon.
iterating over a set of parameter is called a "sweep" in spectre jargon,
or a "parametric analysis" in analog design environment.

try doing spectre -h sweep

to take the input from a file, put the sweep definition in an include file

 

In particular you probably want to create a paramset and then
sweep that. You'd do something like this:

mydata paramset {
a b
1 1
1.5 1
1 1.5
0.8 1.2
....
}

datasweep sweep paramset=mydata {
// analyses within the sweep
tran tran stop=1u
ac ac start=10 stop=1G dec=20
}

Andrew.

 

My problem got solved. Thank you everybody!

Vedank